Hi Geoff,
I forgot to mention that the value knobs also change value in a non-linear fashion with mouse movement speed. If you drag the value knob quickly it will change value at an exponentially faster rate. This is to allow slow careful adjustment while also making it possible to change the value quickly at the same time. Holding SHIFT and moving the mouse quickly can cover the whole range of the Stamp Size value knob in a single motion:
Adding a popup editbox is a neat idea. I will take a look at what needs to be done to make that happen and see if I can squeeze it into the value knob logic. Off the top of my head I imagine that it will probably appear as a little button on the right side of value knobs that you can click to popup a little editbox for typing a knob's value. :]
- Charlie
Hi Russ,
It's definitely tricky trying to invert specific areas. I went ahead and attempted to re-create what you did here and just the design of the card itself doesn't lend itself well to only inverting the diamonds and the area behind them. It definitely requires some fudging stuff around to get those sleeves up!
Personally, I like to V-carve most things with the medial-axis carving operation, maybe even just a shallow cut and fill the rest of the inner areas with the profile milling operation and a Cut Width that reaches the center of large areas with a tiny stepover - or come in with a small flat endmill to clear an area flat.
With the unmodified card image, here's the medial-axis carving operation with a 90deg V-bit down to 0.05" deep:
...and then follow up with a Profile Milling operation with the same V-bit, and a contour Offset of 0.05" to match how far from the edges that the V-carve cut reached in its deepest cuts for a 90deg bit angle, and a 0.015" cut stepover, which could be smaller if I wanted to make the ridges less apparent:
Trying to replicate what you did, with the inverted diamond area, and then I created a Parallel Carving operation with a 0.5mm tapered ballnose, it looks more like the result you ended up with:
I think that it's just not a good strategy to carve something like this as a relief!
Trying again, but using the previous strategy:
It took a little bit of a Smooth factor on the modified raster-layer, and raising the Contour Z on the m-axis carving and profiling operations so they could get good contours, but I think the result speaks for itself! Granted, you won't have varying heights for things, like a relief, but any time there are fine lines it's very difficult to get them to come out nice with something like a parallel carving operation.
Hope this helps! :]
- Charlie
Hi GettingRusty,
Looking good! The main thing to keep in mind is that an image's pixels are interpreted as height values. An image with lighting on it is going to have raised parts where the light is mostly hitting the surface. For example, an image like this:
...results in a canvas like this:
...when you're probably hoping for something more like what originally created the lighting-rendered image, which would be something more like this:
The key is having proper height/depth data if you're using an image, or using a 3D model. Or, if you at least have a black-and-white image you can load it as a raster-layer and trace to a paths-layer and then use Shapes From Paths to generate a 3D shape. You can do the same directly from a 2D vector, like an SVG or DXF that's loaded as a paths-layer. In this instance, you'd want the actual 3D model of the dragonfly from which the image was rendered - that will allow you to generate toolpaths that actually conform to the shape and details of the model itself, effectively turning your carving itself into the 3D model that is naturally "rendered" by surrounding illumination sources. This is what a relief carving is supposed to be.
Having a photograph or lit rendering (like your dragonfly image) is good though if you want to make a halftone or lithopane, but to create a relief carving - a 3D carving of the thing - you'll want a proper heightmap and/or 2D form to generate toolpaths from, or trace to paths that you can then generate 3D shapes from for toolpathing off of.
( EDIT: I thought I'd also include what the actual heightmap for the above example looks like here, just so you can compare with the original image at the beginning of my comment that is only a 3D rendering of this heightmap )
I do think the wood is also of poorer quality than you would want for such a small detailed carving. Of all the woods I've cut so far I've found red oak to be the worst thus, not that I know what kind of wood you're cutting here but it definitely reminds me of red oak's stubbornness. It has really coarse fibers and ends up being very stringy on the edges of cuts. A harder wood like maple or oak is much better for small detailed projects and cuts.
For relief carvings, the best way to go, toolpath-wise, is to use a flat-end cutter with a 2.5D milling toolpath and a Leave Stock that prevents it from exactly approaching the canvas' form. Then come in with a ballnose cutter and a Parallel Carving toolpath with a very small stepover to remove everything else and clean it up. Here is an example project that uses the Rest-Machining option to restrict cuts to the relief carving itself, after removing a bunch of material around it: 5x7x0.5 Deer Relief.pnc Note how the 2D/2.5D milling operations have a smaller border so that more material is cleared, and then the re-roughing/finishing parallel carving operations that employ the rest-machining option are using a different Layer Group that has a larger border so that no vertical cuts are generated at the edges/walls/corners due to using a smaller cutter. We're working on a way to use a paths-layer as a boundary for clipping an operation's cutpaths to in lieu of using the rest-machining option the way that this project does to minimize total cut time.
As long as you have no immediate plunge cuts in your relief, and it gradually enters down into the material with each successive cutpath, you can usually get away with just having a single parallel carving operation and a small stepover that's shaving material with each cut, and as long as you have no vertical walls in the cut while you're using a tapered ballnose it will be fine. Here's an example project where the whole thing is done in one pass that cuts all the way down: 8x8 Tree Of Life 1-Pass.pnc
In a situation where it's unrealistic to do the thing in one pass, it's best to use a 2.5D operation with a larger flat endmill cutter to hog out most of the material, and then come in with your ballnose cutter(s) to go the full depth in one pass afterward.
We're working on getting v1.81b out ASAP right now, which is largely a bugfix update, but the next update we're aiming to include several new features - including some new toolpath types and capabilities! :]
- Charlie
Hi Pat,
No worries, helping people make stuff happen with PixelCNC is all part of the job! ;)
So the canvas Z size is just the maximum potential depth cuts can be generated down to, but if there is content in the canvas volume that is higher than the bottom of the canvas then cuts will only be able to go down to that content with the 3D and 2.5D operation types. So if you want to cut some shapes into the workpiece they will need to be as deep was you want to cut when using a 3D or 2.5D operation. The canvas' Z size is the depth limit you'll be able to have shapes go, and why it's the Max Depth limit (unless the tool's length limits it first, and Ignore Tool Lengths isn't enabled).
With the 2D milling operations the canvas is only used to generate a 2D contour to generate cuts from, regardless of how shallow/deep that contour is generated at, and cuts will always go down to Max Depth.
I believe the reason you're seeing the cuts being offset way into the digits with the 2D offset milling operation is because of your tool definition. It automatically offsets the contour that cuts will be generated inside of by half of the cutter's diameter, where the diameter is the widest part of the flutes (typically the shank diameter for most tapered cutters). We might change this so that it only offsets cuts by the diameter of the cutter at Max Depth, rather than the full width of the cutter.
The 2.5D milling operations properly accommodate for the cutter's geometry at each cutting depth, so with a tapered cutter you will see cuts progress more toward the middle of pockets the deeper it cuts, as it's not able to keep the tool inside the boundary of the shape without moving it away from the edges of the shape at each successive cutting plane, like this:
This is what happens when I generate a 2D offset toolpath with a big fat wide-angled tapered cutter, the cuts must be moved inward to accomodate the full diameter of the cutter:
So if it only cuts that top layer it will never reach the full diameter of the cutter, which is what you're seeing. You can fix this by creating a tool definition that only has a diameter for the depth you plan to cut, but I think I'll be changing it so that it automatically only uses the Max Depth the cutter will go to determine how far to offset the contour for a given tool.
I think the best way to go is make sure that your digits are actually 0.5mm deep and use the 2.5D milling operation instead, to ensure that the tool is always cutting out to the edges for each cutting depth. You can see the depth of your canvas at any point by putting your cursor over the bottom of one of the digits and looking at the XYZ cursor position on the status bar, it will give you a readout of the coordinate (relative to the canvas origin) of the point on the canvas surface that the cursor is pointing to, like this:
This is with the canvas Z size set to 1 inch and the machine origin is at the bottom of the canvas, so with my ampersand being 0.1" deep the canvas surface only varies between 0.9" and 1.0" (from the Z origin at the bottom).
You *might* need to make your digits slightly deeper than 0.5mm, as there can also be a bit of contouring depth precision variance that results in the very bottom of a pocket not getting contoured even though it appears to be down to the Max Depth specified, because numerically it will looks like it's 0.000001mm above -0.5mm, due to floating-point rounding errors that can occur. We did add a tiny Z offset to a few operations' toolpath generation algorithm to mitigate this so you might be fine just making sure your digits are actually 0.5mm deep from the top of the canvas and calculating a 2.5D Offset Milling toolpath with a 0.5mm max depth.
Hope that helps!
- Charlie
